Good morning,
I would like some help trying to solve this problem in my code.
I have a rotation in one of the bodies, and a moment applied in the other. Both of them have a coupling constraint.
I am quite blocked… I have managed to get it to work in Abaqus, and have read the user guide of Calculix to make it work here, but I think I am missing something!
Thank you very very much!
CNIM_66_calculix.inp (2.1 MB)
This is plane stress model. Try excluding DOF 3 from the coupling definition.
1 Like
Thanks @FEAnalyst. I think that was a good suggetsion! The model runned know but stopped in the second increment.
I know get this info messege which I doubt if it means something is wrongly defined with my BCs or couplings¿?
linear MPCs and
nonlinear MPCs depend on each other
common node: 12748 in direction 1 (the sam for 647 in direction 1)
There are many issues and limitations with constraints in CalculiX analyses involving 2D elements. I would try the same setup on a 3D model to see if that’s the problem.
could problem sketch with dimension and force in units provide? result from Abaqus also interesting to compare.
I cannot do a 3D analysis, it has to be 2D and that is the main problem… but I think Iit has to work…
The problem is in this node in the corner.
I have a coupling which involve all the nodes of the border. However I do not know why I get only an error in this node and not in all…
I do not understnad your question. Do you mea if units in the model are ok for dimensions and forces??
I am using mm for dimensions and N for forces and Nmm for torques
I have not looked at your .inp file but generally this happens when there is conflict between two opposing BCs. Can you leave that node out of the selection ?
Use node select to select all the other nodes.
I mean just checking it in 3D to see if it’s CalculiX’s limitation.
The error messages typically point only to the first node with overconstraint so it likely occurs for all the nodes involved in coupling constraint. Unless that node is actually involved in another constraint/BC.
is the question being the same as in CalculiX forum? i replied there clearly.
It’s from this thread: Error solving: SPC meaning - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX).
1 Like
Not sure what you mean! I am asking in calculix corresponding to the same model which I am working, but did not see your clear answer… sorry for that!
yes it continues from previous treads related to kinematic coupling probably.
coupling type kinematic in CalculiX have limitation in force loads of translation dof only i.e no rotational force of moment/torque, boundary rotation still can be. It is not the same as in Abaqus probably and needed to switch to type of distributing in case of moment/torque force, i hope that’s clear.
1 Like
Ok with that.
So from what I understand you are suggesting me to change the constraint of the reference node where I apply the moment to a type distributing.
However, I read this in hte user guide:
No kinematic relations are created between the reference node and the coupling surface, so applying displacement constraints in the reference node has no effect.
In that case would this have sense? Would the displacement (x,y) be blocked??
*Coupling, Ref node=25495, Surface=RBE2_P_CNS, Constraint name=Constraint-pinion
*Kinematic
1,2
*Coupling, Ref node=25497, Surface=RBE2_G_CNS, Constraint name=Constraint-gear
*Distributing
1,6
*Boundary, Op=New, Amplitude=AMP_ROT
25495, 1, 2, 0
25495, 6, 6, 1.01000
25497, 1, 2, 0 ←
*Cload, Amplitude=AMP_TORQUE
25497, 6, 6, 598800
That’s right, for *DISTRIBUTING, you can’t use *BOUNDARY.
for 2D element in CalculiX is not allowed to define MPC in Z direction due to expansion and internal constraint. I’m not yet tested and look further in problem since it’s too large for example, maybe something like this can work.
*Coupling, Ref node=25497, Surface=RBE2_G_CNS, Constraint name=Constraint-gear
*Distributing
1
2
6
p.s coupling type distributing need to change and refers to surface set instead of node set.
Since the differences between coupling constraint types in CalculiX can be really confusing, I summarized them on the CalculiX forum: Different coupling constraints and their limitations - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX).
oh! I did not understand that! I that case @FEAnalyst I should delete this B.C:
*Boundary, Op=New, Amplitude=AMP_ROT
25497, 1, 2, 0 ←
Thnaks for that P.S. @synt. I already changed that and defined Surface "RBE2_G_CNS with elements. I tried with:
*Coupling, Ref node=25497, Surface=RBE2_G_CNS, Constraint name=Constraint-gear
*Distributing
1
2
6
And I got this error. How can I know which is the fatal error?? which is the file to check?
*ERROR in calinput: at least one fatal error message while reading the input deck: CalculiX stops.
The syntax here is the same as for *KINEMATIC:
• first degree of freedom (only 1 to 6 allowed)
• last degree of freedom (only 1 to 6 allowed); if left blank the last degree of freedom coincides with the first degree of freedom.
Repeat this line if needed to constrain other degrees of freedom.
So listing the DOFs one by one in subsequent data lines like this may not work.